开云体育

Hi Alan,

I've read that you DON'T want to center punch the holes for CNC,
although you might want to make light "witness" crosshairs to mark their
location. Best would be to always start with a center drill, then
follow with the appropriate drill. The trouble with a punch mark if not
EXACTLY where you want it, is that it will pull a drill bit off. If the
CNC has moved to the proper location, then you just want to drill where
you are!

To position the mill to a hole's location, set up a "wiggler" in the
spindle, and, using a magnifying glass if necessary, move it tho the
crosshairs. Or, you might prefer to locate everything relative to a
pair of edges (LL corner is often good), and let the CNC work from
that. I like using the edges if it's a new part, and then let the CNC
find the other points.

I'm using Vector CAD/CAM, and if I put a point at each hole location,
down at the depth I need for the center drill, Vector will do a move to
a location ABOVE Z=0, and then a slow Z down to the required depth,
center drilling it for me. It will also generate a following G81 with
the coordinates, which I modify to G83 to actually drill the hole (I
like the "peck" and "dwell"). I "comment out" the G83's with a '/' in
the part program, and turn on "block deletes" on the controller program
(DON'T FORGET!). With the center bit "touched off" in Z, I run the
program with block deletes on. This way, the center drill drills all
the holes I want. Then I replace the center drill with a drill bit of
the required size (you may want to repeat the process with two or more
drill bits), disable block deletes, and run the part program again.
With block deletes disabled, the G83's will be run, and the holes
drilled. OK, this may not work for a "PRO" shop with tool changers and
the like, but it works fine for my Sherline's, and I assume it will work
as well on my RF-31 mill (when I finally get it converted) and possible
a lathe in the future.

HTH

Alan KM6VV
P.S. You can set the Z depth to just "kiss" the stock with the center
drill, and thus run a "verify pass" first, to check your program! Also,
a "pen holder" in the spindle, and a piece of paper can give you
re-assurances that you've programmed the Gcode correctly. I've taken to
printing a 1:1 of the part and the cuts on paper (HP laser is not far
off), and this also helps to verify setup, CLAMPS, etc.

alan@... wrote: